LinuxCNC cutting corners while staright line GCode

More
26 Sep 2013 16:27 #39206 by gaeldk
Hello,

I started an operation to level my table and generated some simple GCODE that basically moves the cutter above the entire surface.

As you can see from the attached screenshot, the GCODE in white is showing straight lines in the corners while the machine is rounding corners as shown in red...

Why is that ?

Thanks


Attachments:

Please Log in or Create an account to join the conversation.

More
26 Sep 2013 17:24 - 26 Sep 2013 17:27 #39210 by Rick G
Take a look here...
www.linuxcnc.org/docs/2.4/html/gcode_mai...#sub:G61,-G61.1,-G64:

Your program probably has G64 set

G64 without P means to keep the best speed possible, no matter how far away from the programmed point you end up.


try adding the line
G64 p.001 q.001
To the start of your program to set the tolerance.

Rick G
Last edit: 26 Sep 2013 17:27 by Rick G.

Please Log in or Create an account to join the conversation.

More
26 Sep 2013 17:36 #39211 by gaeldk
Thank you Rick.

There is no G64 is my program, adding G61 did fix the issue.

How can I tell LinuxCNC to operate with G61 by default without having to manually add it to each program ?

Thanks

Please Log in or Create an account to join the conversation.

More
26 Sep 2013 17:51 - 26 Sep 2013 17:53 #39212 by Rick G
You can add it to your ini file.

www.linuxcnc.org/docs/devel/html/config/...b_rs274ngc_section_a

Depending on what you are doing you may not always want to use G61 as very short lines can cause slow stop and go motion,

There is no G64 is my program


It is normal for it to be the default.

Rick G
Last edit: 26 Sep 2013 17:53 by Rick G.

Please Log in or Create an account to join the conversation.

More
26 Sep 2013 18:11 #39215 by andypugh
That degree of corner rounding seems to indicate a miss-match between the machine speed and the machine acceleration limits.
Have you tried much higher acceleration? How did you determine the accel limits?

Please Log in or Create an account to join the conversation.

More
26 Sep 2013 19:58 - 26 Sep 2013 20:00 #39219 by BigJohnT

Thank you Rick.

There is no G64 is my program, adding G61 did fix the issue.

How can I tell LinuxCNC to operate with G61 by default without having to manually add it to each program ?

Thanks


It is good practice to not assume the state of your machine when you run a G code file. A preamble line that sets the environment is normal. You can never tell what state the last G code program left your machine in.

gnipsel.com/linuxcnc/g-code/gen01.html

Also please read and understand what M2 does.

linuxcnc.org/docs/html/gcode/m-code.html#sec:M2-M30

JT
Last edit: 26 Sep 2013 20:00 by BigJohnT.

Please Log in or Create an account to join the conversation.

More
28 Sep 2013 15:48 #39304 by gaeldk
Acceleration is set to 60 mm /s2 and velocity to 34 mm / s

Have no idea how this has been calculated by the provider of my router (cnc4all)

Will look at how to calculate acceleration...

Please Log in or Create an account to join the conversation.

More
28 Sep 2013 17:08 #39311 by gaeldk
I played with the stepconf configuration and my machine can take up to 1000 mm s2 :S ?? Of course then the movements are very brutal...

So between 60 and 1000 I have no idea whatsoever what a good acceleration value is...

All I know about the steppers is 1,7 Nm 4A ... 1600 steps/rev

Please Log in or Create an account to join the conversation.

More
28 Sep 2013 17:51 #39313 by Rick G
section 5.1.2 of stepconf manual has a test procedure for acceleration.
You do need to error on the cautious side to avoid missing steps, especially when actually cutting or under load.

Rick G

Please Log in or Create an account to join the conversation.

More
28 Sep 2013 19:00 #39315 by andypugh

I played with the stepconf configuration and my machine can take up to 1000 mm s2 :S ?? Of course then the movements are very brutal...
So between 60 and 1000 I have no idea whatsoever what a good acceleration value is...


Somewhere between where you get the path-following you want and where the machine either loses steps or shakes itself apart.

Accel numbers tend to be 10x to 20x the velocity number. But it is a compromise and depends on the machine.

Please Log in or Create an account to join the conversation.

Time to create page: 13.238 seconds
Powered by Kunena Forum